Exporting .DXF/DWG Files from SolidWorks....?

[mcb79]

I am interested in purchasing Solidworks, for its great design capabilites, and also it's sheet metal module.
Will I be able to import an .acis file of a 3d steel connection, then unfold it in solidwroks, and from there, export the unfolded part as a .dxf/dwg file?
I need the unfolded part in 2d dxf/dwg format in order to nest it.
Is this possible with solidworks...?

Thanks for the help.

 

[josephv]

Hello,

Yes, you can do this in SolidWorks.

As you said you can unfold the part. You then create a drawing of the unfolded part and do a Save As DWG/DXF.

cheers,

Joseph

 

[Arlin]

Yes, you can quite easily import a solid sheemetal part model and flatten it in SWX.

A couple things to keep in mind though:
1.) The Solid Model must have a constant thickness.
2.) The Solid Model bends must all be either cylindrical or conical.
3.) The Solid Model must be able to be flattened. For instance, you cannot flatten an orange peel.

 

[mcb79]

Thanks for your replies. You have been a great help already.

Once I have exported the file as a .sat file.
Solidworks opens it as a .sldprt file type.
How do I make it into a drawing file so that I can "save as"
dxf/dwg while the part is in its folded state? I can not save a .sldprt as a dxf. The option is not available.Also, everytime I attempt to "save as", I am prompted to fold the part. I need to export into dxf so that I can nest the part with it's scrible line at the bend point.

Mike

 

[TheTick]

For dwg/dxf, you need to make a drawing (*.slddrw) of your part and export from there.

Someday, someone may kill you with your own gun, but they should have to beat you to death with it because it is empty.

 

[TheTick]

Forgive me if this is too pedantic....

SolidWorks drawings are files separate from parts or assemblies. There is a tutorial in the help section which will tell you how to put model views into a drawing.

The simplest way to put a part into a drawing is drag-and-drop the file into the drawing. This may or may not give you the orientations you prefer. For more control, investigate the "Insert-->Drawing View-->Relative to Model" method.

Someday, someone may kill you with your own gun, but they should have to beat you to death with it because it is empty.

 

[mcb79]

I must be losing my mind here!
When I open a .sat file, and insert my bends, then attemot to "save as" first I am prompted to fold the part. Then I go to save as, file type, and there is no option to save as slddrw. Does anyone know why I dont have this option?

 

[jdsmi]

You will need to open a new drawing (.slddrw).

Drag the model you just imported (.sldprt) into the new drawing window then do a "save as" from the drawing.

 

[mcb79]

Hey Tick, Great tip with the drag and drop. That is really cool. I am messing around with this on a friends PC and it is looking pretty good...Only problem is that when I drag and drop, it only gives me a top, front and side view of the part in its folded state. Is it possible to drag and drop, and obtain a view of the part in a folded state?
Im getting there. Thanks for the help sp far!

Mike

 

[TheTick]

investigate "Insert-->Drawing Views-->Relative to model"

This is where you can orient a drawing view relative to an object's faces.

After that, use "Insert-->Drawing View-->Projected" to get any desired projections.

Someday, someone may kill you with your own gun, but they should have to beat you to death with it because it is empty.

 

[Arlin]

First, I will give you a crash course in SWX, sheetmetal, and configurations.

SWX has 2 different sheetmetal modes: 1-create a sheetmetal part by first begining with a solid part or 2-Create a sheetmetal part by using sheetmetal features.

Since you are importing a solid and turning it into a sheetmetal part, you are using the first method. (I say this because the two methods vary fairly significantly).

After imorting, you simply "Insert Bends." This will convert your solid into a sheetmetal part that can be flattented (if possible).

At the bottom of the feature tree will be a "process bends" feature. Now, that feature does exactly what it says, it processes the bends in your model. So, when it is unsupressed, the part is bent and when that feature is suppressed, you will get the flat pattern for your part.

I assume you have been flattening you part by dragging the red bar above the Process bends feature. Solidworks will not let you save the part unless the process bar is at the bottom of the part.

Enter configurations. If you make a configuration of your part, you can suppress the Process Bends feature in one config and leave it unsupressed in another config, giving you a default and a flattened model.

You can create the 'Flat Pattern' configuration automatically by going to your drawing, selecting Insert View, selecting your model, then selecting "Flat Pattern" from the list of views that come up. This will automatically create a Flat Pattern config in which the process bends feature is suppressed and add that view to your drawing.

Hope that was enough to get you going.

 

[SWMNKY]

We have trouble when exporting drawings to DXF. Even with "Hide All Types" selected, the dxf has bend lines as well as any construction sketches on the part.

How can we automatically hide these without right-clicking each sketch and bend line?